Welcome to the Frequently Asked Questions (FAQ page). Below, we have tried to answer the most common questions we hear from 5Spice users.

updating 5Spice 2.0Registered users should install 5Spice 2.70 (or higher) now to allow registering 5Spice on new computers in the future. See FAQ 4Get the latest features and bug fixes!

Blocked simulation, no error message, bug (version 2.00-2.31)Adding a schematic symbol that links to a model (diode, FET, subcircuit, etc.) and then not linking the symbol to a model AND not connecting the symbol with wires, blocks simulation from starting. This is a bug. There is no error message.

Occasional problem with multi-page schematic not fully drawing when loading from file?(Pro versions up to 2.62) update to current version.

Diodes Inc models 2015-2016The company continues to release model files with ever more .Subckts missing the critical .Ends statement. Update to version 2.60 to avoid many missing models in the 5Spice model selection lists. Even with 2.60, still recommend avoiding the All-In-One file.

29. How do I model a transformer with center taps on each winding? Or add another winding?

30. How do I use User Defined Parameters to set and sweep multiple component values?

1. No more program registration for new users! Existing registered 2.0 users OK.

As the 5Spice business is closing, it is no longer possible for new users to register the program. This means the advanced features are not available to them.

Registered 5Spice 2.0 users: 5Spice versions 2.70 and up allow you to register 5Spice on a new computer (or a re-install of Windows) without entering a Transfer code obtained from Andresen Software. This will allow you to continue to use the program after the business closes.

Registered 5Spice 1.0 users: you can install and use 5Spice 2.0 but registration is not available. This means the features unlocked by registering 1.0 will not be available in 2.0.

2. Can I install 5Spice without un-installing an earlier version 5Spice 1.xx?

Yes. Newer 5Spice is a separate program. The install program installs it in a separate directory. Both programs can run at the same time if you want to compare results.

3. Can I install 5Spice on top of an earlier version 5Spice 1.xx?

Not recommended. 5Spice now is a separate program from version 1.xx. Please allow the install program to install 5Spice in a separate directory.

4. I installed a new operating system and my registration code no longer works. or How do I transfer the registration to the new system?

Registered (paid) users of earlier versions of 5Spice 2.0 should download version 2.70 or higher. See the instructions in the Registration dialog for how to enter your registration information.

If you can’t find your original registration email, you can try to contact Andresen Software. However the business is closing so sometime in 2019 that will no longer work. Contact Share-it (the original seller) to obtain a copy of your original license email.

5. How do I transfer my customized settings and Library to a new installation of 5Spice?

User preferences/optionsare stored in file 5Spice.ini. You may copy this file to the new installation of 5Spice by overwriting the existing file while 5Spice is not running. See main menu TOOLS>Location_of_5Spice_Files for file location.

Library (see main menu TOOLS>Update/Rebuild Spice Model Library for location)Any model files you added to the Library can be copied to the Library of the new installation.

Any Pin Connection information you added for subcircuits (models) is stored in file _User.PIN in the 5Spice Library folder. Copy this file to the new installation’s Library folder.If you have already added Pin Connection information in the new installation, you can combine the contents of the old and new _User.PIN files using a text editor. Please avoid duplicate entries.

6. Can I use 5Spice in countries where numbers are written differently than in English?

The data entry fields accept numbers in the national style that Windows is set for. But there are limitations. The program will not work where Windows displays a negative number as 12- or (12). Non-English alphabet characters may not be used in component reference designators, node names, numbers or anything else that is part of a netlist (circuit description).

Model and Subcircuit files you add to the Library must conform to Spice standards: non-English characters allowed only in comment lines, numbers written as 1.23 (never as 1,23).

7. Does 5Spice support users new to circuit simulation?

If you have never used circuit simulation before, you can still create a schematic and run a simulation. But you probably need to know what is covered in a circuit analysis course to understand what is going on in the various types of analyses. And read at least some introductory articles on Spice circuit simulation. 5Spice has a brief description of each analysis type - see the Help index. Also be sure to read Introduction and Simulation and Circuit Design in the Help section of the main menu.

8. After running DC Bias analysis, I don't see the node voltage pop up when I position the mouse over wires in the schematic?

Information should always pop up when the mouse is positioned over wires and components. For wires, the node voltage should pop up after running DC Bias. A user with a Logitek mouse reported a problem where the pop ups were mostly missing. Installing the latest mouse driver fixed the problem.

Also remember that editing the schematic causes the node voltages to stop displaying (their value may have changed). Look on the DC Bias page for the results or run the analysis again.

9. How do I select an analysis other than DC Bias, AC and Transient?

In the form where you select which analysis will run (Analysis Dialog), press the “Add Analysis” button.

10. What type of processor(CPU) will give the fastest simulation?

All processors now have multiple cores. While simulating, 5Spice 2.0 uses one core fully and partially uses a second. So the most important specification is clock speed, not number of cores. For very large circuits or processors with small on-board memory caches, the speed of the memory on the motherboard is also important.

We recommend a dual or quad core processor with the highest clock speed. Most dual cores run faster than processors with more cores because there are only two cores dissipating heat. If you look at a processor with more than 4 cores, make sure it has more than one floating point math unit for all the cores. Spice and 5Spice spend most of their time doing floating point math.

Be aware that Intel and AMD sell lower cost processors with simplified architectures that reduce performance (slow...) even though the clock speed may be the same as a more expensive model. Buy the more advanced architectures and avoid the lower cost models.

As of 2016, an Intel Core i3 or i5 makes a powerful Spice simulator.

Processor Speed RestrictionSurprise, Windows restricts your processor’s maximum clock speed, especially in a laptop but also on the desktop. Go to Control Panel > System > Power Options to see basic choices. For details, see processor power management in “advanced power settings”

11. When I export the schematic to an image file, part of it is cut off?

The image file captures what you see of the schematic. Zoom out until you can see the entire schematic before exporting. However only part of the largest schematic size will show with full detail. You can copy a section in 5Spice, create a new, smaller sized schematic, then paste and export.

12. What schematic symbol to use for a Darlington transistor?

Use the symbol for an ordinary bipolar transistor.

13. I can't find the right schematic symbol for my subcircuit?

5Spice does not have a way for the user to create new schematic symbols. However you can use the generic subcircuit symbol for any subcircuit whose .Subckt definition line lists between 2 and 100 nodes. This symbol looks like a rectangle with pins along its sides. It is located in the parts toolbar next to the OpAmp symbol (5-9 nodes).

You link either symbol with your subcircuit by editing the symbol. The symbol will then adjust its number of pins to match the number of nodes in the subcircuit's .Subckt definition line. You can also add names to the symbol's pins.

14. Why doesn't the subcircuit symbol have the same pin numbers as my favorite device package?

Spice knows nothing about pins, packages or schematics. What you see on a Spice .Subckt definition line is a list of circuit nodes that connect externally. This is a universal way of connecting a circuit.

.SUBCKT subckt_Name nodeA nodeB nodeC .....

The circuit nodes are identified by a name or a number. If numbers, the subcircuit's author may or may not have assigned numbers matching the pin numbers of some particular physical package (Spice has no standard).

In 5Spice we work directly with the node numbers/names since that is the only thing that is consistent across all Spice subcircuits. This allows you to add any subcircuit to the Library.

The program connects the nodes to pins of the schematic's rectangular subcircuit symbol in the order the nodes appear on the .Subckt line. The first node (nodeA in example) always connects to the symbol's pin s1, no matter what the node's number/name is. The second node (nodeB in example) always connects to pin s2. And so on.

You can add your own descriptions to the subcircuit symbol's pins to eliminate confusion. Usually the author has added comments near the .Subckt line describing the circuit function of each node. To add descriptions to pins: edit the schematic symbol, select the subcircuit, press the Add Connection Information button. Descriptions are saved in the Library.

So just ignore physical package pin numbers when working with 5Spice.

15. How do I add models and subcircuits to the Library?

See the program’s main menu > HELP > Spice Library

and main menu > TOOLS > Update/Rebuild Spice Library

16. I added files to the Library but do not see the models/subcircuits when I edit the symbol in the schematic.

Check that the files are in the correct part of the library. Models and subcircuits that link to schematic symbols of diodes, transistors, FETs (all types), IGBT, SCR and TRIAC go under the DIODE_BJT_FET section. All others go under the SUBCIRCUITS section.

Windows Explorer in Windows 7, 8, 10 shows the contents of ZIP files as if they are extracted when they are not. You must extract the files manually.

After adding files or changing subcircuit names, you must rebuild the Library index. Go to main menu TOOLS and select Rebuild Library.

If a subcircuit contains model types not normally used to model the symbol, 5Spice will not display that subcircuit in the list when editing the symbol. To show the subcircuit in the list, edit the symbol and uncheck the box that says "only show matching subcircuits".

5Spice can't recognize a model or subcircuit if the period is missing from the start of the .Model or .Subckt line. It may not recognize a model if there is a major syntax error before the first parameter in the .Model line.

5Spice does not recognize files ending in .TXT (as in "readme.txt"), .BAK, .DOC, .EXE, .HTM, .HTML, .SAV or .ZIP as library files. If a Spice file has a .TXT extension, change it to .MOD or some other extension.

If you open a model file in a word processor or browser and then save it, hidden formating characters are often inserted into the file which can confuse any Spice program. Either use Windows NotePad for editing or use SaveAs and save the file in text format. Windows NotePad will add a .TXT extension to the file name when it saves the file unless you select the *.* filter before saving.

>Note that Windows hides the .TXT file extension by default. Change this in Windows folder settings by unchecking “Hide extensions for known file types” .

17. I added MOSFETs to the Library but do not see them when I edit the symbol in the schematic? (or if I uncheck the "only show matching subcircuits" box and select the MOSFET, I get a "too many parameters" error from WinSpice when I run the simulation.)

There are two classes of MOSFETs and thus two classes of MOSFET schematic symbols. Spice handles each differently.

Power MOSFETsIf you are not designing an integrated circuit, it is almost certain that you are using power MOSFETs, not simple MOSFET transistors. IRF, On Semi, ST and most others make power MOSFETs. Unlike simple MOSFETS, power MOSFETs contain a body diode and are modeled using a SUBCKT statement in Spice. Use the power MOSFET symbol in the schematic - it shows the body diode.

Power MOSFETs with thermal modelingSome power MOSFET subcircuits include thermal modeling and thus have 4, 5 or 6 terminals (nodes), not 3. 5Spice includes a 5 terminal MOSFET symbol for thermal modeling.For subcircuits with 4 or 6 terminals (nodes), use 5Spice‘s rectangular subcircuit symbol.

simple MOSFETsIf you are designing an integrated circuit, then use the simple MOSFET symbols in the schematic. Also use these symbols for small signal MOSFETs like those used in RF receiver amplifiers, charge amplifiers or with the sensor in a smoke detector. These symbols work with MOSFETs that are modeled using the Spice MODEL statement. The 4 terminal symbol will also work with a 4 terminal subcircuit that contains a simple MOSFET.

18. How do I make a 5Spice schematic into a subcircuit?

The Professional level of the program includes a tool to automate this process and track revisions.

19. What important parts of my circuit are not modeled by Spice?

Two important parts are the power supply impedance and the ground layout and impedance.

Spice voltage sources are often used as power supplies when simulating. These have either zero impedance or, in 5Spice, a 1E-3 ohm resistance. Therefore you will not see the dc drop or the power supply noise that will be present in the physical circuit. (noise due to changing supply currents).

You can model the power supply impedance for more accuracy. But subcircuits that model op amps and other devices almost never model the device’s power supply rejection over frequency. Only a physical circuit will give this information.

Ground impedance issues are more complicated and can determine the success or failure of a design. Spice’s ground symbol provides the perfect, zero impedance connection between all points. No real circuit or ground plane is like this. For an in depth discussion of ground currents and grounding, see this article.

20. DC Bias fails with my feedback circuit no matter what I do?

Spice computes the dc operating point before running any analysis. A circuit that has digital output levels and feedback to make it oscillate may not have a stable dc operating point. This will cause 5Spice to fail in DC Bias.

To run a Transient Analysis on the circuit:If the circuit uses resistor-capacitor feedback or an RC charging circuit, you force the dc operating point during Transient analysis by adding an Initial Condition symbol connected to the capacitor. Otherwise you must modify the circuit so it is dc stable during DC Bias but not during Transient Analysis.

Example: A 5Spice digital logic invertor is an ideal logic gate. Its output is defined by an IF-THEN statement and can only be high or low. If its output is connected to its input with a resistor and capacitor to ground, there is no stable dc operating point. DC Bias and all other analyses will fail.

1. Add an Initial Condition to the schematic, wire to the IC to the capacitor. Set the IC for any voltage and enable Initial Conditions on the Transient Analysis setup page.

OR

2. Modify the circuit by adding a voltage controlled switch that is controlled by a separate Signal Source. Set the Signal Source to the STEP waveform. Then the switch will be in one state for DC Bias and TIME=0 of Transient Analysis and in the other state during the rest of Transient Analysis. Connect the switch to the circuit as necessary. In this example one could short the capacitor.

(Note: this is not a practical circuit since there is no hysteresis at the input of the invertor. The simulated circuit may or may not oscillate when the voltage on the cap reaches the invertor's input threshold - depends on the values used to set up the analysis and on numerical round-off in Spice.)

21. How do I graph power, log() or some other calculated quantity?

Graph Plot Equation

You can enter an equation to calculate a graph Plot from the data of one or more TestPoints. TestPoint data may be modified or combined with math operators, functions or the power function (PWRdiss). In AC analysis the Relative Phase function (RelPhase) is also available.

See details by pressing the Edit button on the Graph/Table page of the program’s Analysis Dialog

POWER: Place a Voltage and a Current TestPoint in the schematic. Enter an equation on the Graph/Table page using the PWRdiss function to calculate power from the data of the two TestPoints.

Multiplying a voltage TestPoint times a current TestPoint usually does NOT give correct power dissipation in AC analysis. Complex math uses the absolute phase of both numbers but power dissipation requires the relative phase. Use the PwrDiss function, which works in all types of analysis. Its AC power output is always positive to allow display of power in dB.

If you want the V*I product instead of power in AC analysis, use the multiplication operator and select Magnitude display in the graph.

NonLinear Source method

You can use the NonLinear Source to implement an arbitrary math equation in all types of analyses. The schematic symbol is a rectangle saying Fxy. In AC and Noise Analysis, the NonLinear Source linearizes its equation if it is nonlinear - which gives the user unexpected results.

Add a copy of the program's NonLinear Source to the schematic (use the version with voltage output). Then edit it to enter the equation you want. Connect the source's inputs to your circuit. Connect a TestPoint to the source's output and graph the TestPoint.

POWER (does not work in AC or Noise analysis): Connect the desired circuit voltage to one input, say X. To calculate power you also need a current. Add a current controlled voltage source to the schematic and use it to convert the desired current to a voltage. Connect this voltage to the Y input of the NonLinear Source. Use both inputs in the power formula: X*Y

Working with switchers is one of the trickiest things to do with Spice. A good book may help (see link to Basso's website on the Links page for one possibility). Here are three common problems.

the rise time surprise (sooner or later it will bite you. 5Spice prevents most cases.)

People often use Spice's Pulse waveform generator to get the switching waveform/clock for their circuit (in 5Spice this is in the Signal Source component). For the Pulse, Square Wave and Exponential waveform generators, Spice uses the TimeStep value for rise or fall times if you don't enter a value for them or enter zero. In this case, a large TimeStep relative to the pulse's width will give dramatically slow rise or fall times, affecting the turn on/off times or duty cycle in your circuit.

A further surprise occurs if you also don't specify the TimeStep value. Spice defaults to TimeStep = simulation run time / 50. Now when you change the simulation run time, the TimeStep varies and therefore the rise times also vary.

ALWAYS specify your rise times. NOTE: 5Spice requires users to enter rise times for pulse and exponential waveforms. For square wave with no rise time specified, 1/100 of the square wave period is used.

A reasonably fast rise time also helps Spice synchronize its computation points with your switching clock edges which is important for accuracy. See next paragraph.

the Spice TimeStep gremlin

Spice computes a solution at least once per TimeStep. Look at the TimeStep you specified for the Transient Analysis and compare it to the switching frequency you are using. As an example, say you switch at 100KHz and set the TimeStep to 5usec. At a 50% duty cycle, the switch is both ON and OFF for 5usec. If Spice had only one computation point during the switch ON (or OFF) interval, it couldn't tell how the current in the inductor is changing over the interval. So Spice adds a few more computation points automatically. But the algorithm it uses is not directly aware of your constant switching frequency - so you may not end up with a consistent number or spacing of data points in each switching cycle. Which can lead to wandering or uneven graph plots.

To prevent this, use a reasonably fast clock rise time somewhere in the schematic. This helps Spice synchronize its computation points with your clock edges. Clock the circuit synchronously with the Pulse waveform (5Spice's Signal Source component) rather than using a self generated clock. Spice pays special attention to circuit transitions that occur just after pulse waveform transitions.

ALWAYS use 5Spice's "fine" setting for the dynamic TimeStep (set TRTOL=1 in other simulators). This increases the number of automatically added computation points in areas where the waveform is changing. It may sometimes also be necessary to set the TimeStep to force 5-10 or more computation points during the shorter of the switch ON and OFF intervals.

These settings can result in very long simulation times. You can try the SMPS convergence option which speeds simulation up at the cost of lower accuracy. Or you can look at the small signal behavior (step response) with a formula (based on the switcher circuit topology) which simulates much faster - see link to C. Basso's models. This would be done in a separate schematic. Then in the original schematic you add an initial condition on the output capacitor to set it to its final voltage (Initial Condition symbol for schematic) to shorten the startup time of the full switcher circuit. And study steady state switching waveforms with the full circuit and a very small TimeStep.

numerical oscillation of the Integration method

After you have followed the guidelines above, note that Spice's standard integration method is not always numerically stable. This can show up when there is a time constant shorter than the TimeStep (often true in switcher semiconductors as junctions turn on and off). The math can oscillate numerically. This is normally visible in the graph but in a switcher it may be confused with switching noise. This numerical oscillation can possibly beat with your circuit's switching frequency, causing low frequency effects. Try selecting the GEAR integration method which is numerically stable and see if results change. Gear can have overshoot spikes on fast rise time edges so you can also try the Backward Euler integration method. Of the three methods, Backward Euler is the slowest and has the most error buildup over long simulations.

In AC analysis, Spice linearizes all the nonlinear circuit equations including your formula. It does this by taking partial derivatives at the circuit's DC OPERATING POINT. Spice uses the derivative it computes from the formula as the proportionality constant or "gain" of the NonLinear source during AC analysis.

When calculating the derivative, the source’s X and Y inputs (X and Y in the formula) are set to the dc voltage determined by the dc operating point of the circuit.

This can lead to surprises when X or Y are used in the formula and one or both of their dc operating points is zero!

Formula Examples:

1. Fxy = 1.0, the derivative of a constant is always zero. So the output is always zero in AC analysis.

2. Fxy = 1.0*X, the derivative = 1.0 as expected. No surprise here.

3. Fxy = X*X and the dc voltage of X is zero. The derivative is zero: in the limit as X goes to zero, for a very small change in X around zero, the output is zero. Note the output is going to zero much faster than the input: 1E-100*1E-100 = 1E-200.

4. Fxy = X * Y and both X and Y dc operating points are zero, then the derivative with respect to X, d(Fxy)/dx, is zero since Y is set to zero! And the same for d(Fxy)/dy since X is set to zero. So

Vout = X * d(Fxy)/dx + Y * d(Fxy)/dy = 0

for all values of X and Y.

The same AC behavior occurs during Noise analysis.

More: If the circuit's dc voltage across X is zero AND you add a 1.0v DC source in series with the X+ input to the nonlinear source, you will get the derivatives we tend to expect from math class. This happens since the partial derivatives are now evaluated numerically around X=1v instead of X=0v. But if X does not have a dc value of 1v, you have to think carefully to know what the derivative will be.

24. How do I fix the Transient analysis "time step too small" error?

See the "Simulation Failure" topic under Help in the Main Menu and look for the error name.

25. How do I set the initial current for an inductor or transformer winding in Transient analysis? How do I limit the current?

Spice does not allow setting initial current unless you also set the initial voltages for all the circuit nodes. This is not practical and 5Spice does not support this option. But you can often set the initial current indirectly.

First, remember that Spice performs a DC operating point (DC Bias) analysis using the TIME=0 value of the SignalSource waveform before doing Transient Analysis. So the circuit is 'live" in the DC sense at TIME=0 when Transient Analysis starts.

Reducing Initial CurrentYou can add a voltage controlled switch in series with a inductor/winding and use its resistance to reduce the current through the inductor/winding.

Set the switch’s OFF resistance to limit the current to the desired value. Connect the switch's control inputs to a Signal Source and set it to generate a voltage step at TIME=0. The STEP waveform's amplitude is zero at TIME=0 and non-zero for TIME > 0. Set the switch's threshold so it will be open (off) at TIME=0, then close (on) when TIME > 0. Use a low enough value of switch ON resistance to not disturb normal circuit operation, but not lower than 1E-3 ohms unless you run the Project Wizard.

Setting Initial Current to ZeroAdd a SignalSource in series with the inductor/winding. Set it to generate the STEP waveform. Adjust the polarity and amplitude of the STEP waveform to cancel the TIME=0 voltage across the inductor/winding.

26. How do I create a custom input signal in Transient analysis? How do I model the staircase waveform of a D/A convertor?

You define a PWL waveform by a series of (Time, Value) data points. The first data point must be at TIME=0. Spice linearly interpolates the waveform's value between data points. See program help for details.

How do I simulate the output waveform of a D/A convertor?

Use the PWL waveform. You can model the staircase output of a D/A convertor by defining data points at the beginning and end of each step. The time between steps is the inverse of the D/A clock rate. The time between the end of one step and the start of the next step corresponds to the rise time of the D/A convertor. Spice has trouble with very abrupt transitions so make this time a realistic value. Or do not include rise time in the PWL waveform and use an RC network on the output of the Signal Source to give the waveform a reasonable rise time.

How do I make the waveform repeat?

The waveform will repeat automatically. Look up PWL in the program’s help for details.

27. How do I create a time varying resistor in Transient analysis?

Use the current output NonLinear Source to implement a time dependent resistor. Connect the source's X differential input to sense voltage at the source's output terminals. Get the polarity right or you have a negative resistor.

Then the source's formula is based on I = V/R

I = X / (Rt_value * TIME + R_constant)

where X is a variable that is the voltage at the source's X differential input. TIME is a predefined variable = the elapsed simulation time in seconds during Transient analysis.

Note: you do not enter the "I =" part of the formula in the source's formula box.

28. How to plot I versus V curves for diodes, transistors, etc.?

Use DC analysis. Load the demo schematic “DeviceCurves” to see how.

The Professional level of the program includes X-Y graphing which allows a prettier way of doing this. See the demo schematic “DeviceCurvesPro”, available in 5Spice v2.61 and up.

Registered users could also auto-export the data from Transient or DC analysis, then load the data into a spreadsheet and plot the data there in X-Y format.